CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

Type of boundary condition on the wall

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree8Likes
  • 1 Post By DnyanMiri
  • 1 Post By vinerm
  • 1 Post By DnyanMiri
  • 1 Post By vinerm
  • 1 Post By DnyanMiri
  • 1 Post By vinerm
  • 2 Post By vinerm

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 18, 2020, 06:12
Post Type of boundary condition on the wall
  #1
Member
 
Dnyanesh Mirikar
Join Date: Jul 2019
Posts: 35
Rep Power: 5
DnyanMiri is on a distinguished road
I want to calculate the heat flux removal from a moving hot surface due to spray cooling. What thermal boundary condition should I give to the surface where I want to calculate the surface heat flux?
Heat flux, Temperature or coupled or anything else?

I am giving 0 heat flux boundary condition at the wall and while initialization assigned temperature(1053K) to the surface, am I doing it right?

Please give your valuable opinion. Let me know if you need any more info. Thanks in advance.
Phanindra Raavi likes this.
DnyanMiri is offline   Reply With Quote

Old   February 18, 2020, 07:46
Default BC
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
If you wish to determine heat flux then applying heat flux doesn't make sense. You need to either apply a temperature or convection. For that, you should know the condition at the wall.
Phanindra Raavi likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 19, 2020, 06:40
Default
  #3
Member
 
Dnyanesh Mirikar
Join Date: Jul 2019
Posts: 35
Rep Power: 5
DnyanMiri is on a distinguished road
Thanks for the reply, Vinerm. Yes, I accept my mistake, it shouldn't be an adiabatic wall. The temperature boundary condition in the fluent means constant temperature, right?
In my case, the plate is initially at 1053K and after spray cooling, I want to calculate heat removal from the surface. I'm not understanding what should be my thermal boundary condition at the surface. I cannot give convection as I want to find the 'h' value from the heat flux. Do I need to write UDF for this? If you could give me any advice, I would be grateful.
Phanindra Raavi likes this.
DnyanMiri is offline   Reply With Quote

Old   February 19, 2020, 06:50
Default Two sides
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
Though usually the thickness of the wall is not modeled or simulated, there are always two sides of a wall. So, you need to provide either a temperature (this would not be appropriate for your case) or convection condition (appears to be more appropriate for you). Fluent calculates convection on the side being included in the domain, such as, upper side if water is on top of the plate. But the bottom side is open to the atmosphere. So, you can provide a h value and a T value.
Phanindra Raavi likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   March 4, 2020, 09:56
Default
  #5
Member
 
Dnyanesh Mirikar
Join Date: Jul 2019
Posts: 35
Rep Power: 5
DnyanMiri is on a distinguished road
Thanks, Vinerm for replying back and sorry for the delay in replying. I've probably found out the right condition for the wall. As there is fluid-solid interaction, I have used it as a coupled wall temperature boundary condition. After initializing, using the patch I have given the initial temperature of the wall which is 1053 K.

This probably requires a new thread but still, it is related. I'm using ANSYS 18.2. When I use spray for cooling the plate/wall, at high temperature like 1053 K film boiling takes place. As the temperature decreases, it moves into transition then nucleate boiling regimes. I read through some related literature, I've found out 'wall jet' DPM boundary condition is used for simulating film boiling. Then lagrangian film model for nucleate boiling. I don't understand how to change between these two boundary conditions while simulation.

If you need any more info, please let me know.
Thanks and Regards,
Dnyanesh.
DnyanMiri is offline   Reply With Quote

Old   March 4, 2020, 10:18
Default Droplet in DPM
  #6
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
That's good. As long as walls are coupled, you don't need to do anything.

For DPM, Wall-Jet boundary condition is nothing but an extension of reflect. It only models the momentum of a droplet hitting a hot wall, such as, droplets jumping on hot plate due to Leidenfrost effect. Wall jet model has no mass transfer mechanism.

Wall-Film on the hand provides you multiple options, including mass transfer. I have not checked in the newer version, however, until 16, there is no nucleate boiling option for droplets. For mass transfer, excluding reactions, evaporation and boiling are the only options. It is quite possible that you are referring to boiling and not nucleate boiling. Actually, nucleate boiling phenomenon may not even take place in a droplet because it is too small for a vapor bubble to form. So, most likely, you can use vaporization and boiling. This does not require any extra code or effort. Option is available within Fluent and switches automatically based on the input data.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   March 4, 2020, 13:18
Default
  #7
Member
 
Dnyanesh Mirikar
Join Date: Jul 2019
Posts: 35
Rep Power: 5
DnyanMiri is on a distinguished road
Thanks a lot for the insights, Vinerm. This will help me move forward in my project.
I've found following paper which is closely related to my work, just incase if you want to refer
https://doi.org/10.1016/j.ijheatmass...er.2019.06.098

Thanks and Regards,
Dnyanesh
Phanindra Raavi likes this.
DnyanMiri is offline   Reply With Quote

Old   March 5, 2020, 08:08
Default The Article
  #8
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
It appears to be a good article, however, has mistakes in their representation, at least, if not in their understanding of the phenomenon. But what this paper shows is certainly doable using Wall Film model.
DnyanMiri likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   May 30, 2020, 09:23
Default
  #9
Member
 
Dnyanesh Mirikar
Join Date: Jul 2019
Posts: 35
Rep Power: 5
DnyanMiri is on a distinguished road
Hi Vinerm,
I'm right now stuck at a stage where the problem could be of meshing or implementation of the wall film model.
When droplets reach the surface, after a few iterations I get divergence in turbulent viscosity as well as temperature.
Could you help/advise on this problem? Thanks in advance. I can share the required files.
DnyanMiri is offline   Reply With Quote

Old   May 30, 2020, 14:34
Default Divergence
  #10
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
It could be due to multiple reasons. First of all, droplets should be much smaller than cell sizes in terms of volume. Secondly, the values of the sources terms added to the continuous phase depend on the mass of the particles. If the mass being injected or reaching a surface is very high, it could lead to very high value of source term leading to convergence issues and eventually to divergence. You can plot source terms in Contour plots. Check for their variation as the simulation proceeds. If those values increase all of the sudden, then it could be numerical issue. However, if those increase gradually, then you may try with reduction in the mass being injected.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   May 31, 2020, 01:42
Default
  #11
Member
 
Dnyanesh Mirikar
Join Date: Jul 2019
Posts: 35
Rep Power: 5
DnyanMiri is on a distinguished road
Thanks for the quick reply. I'll ensure these things are taken care of and see what happens.
DnyanMiri is offline   Reply With Quote

Old   June 7, 2020, 12:11
Default
  #12
Member
 
Dnyanesh Mirikar
Join Date: Jul 2019
Posts: 35
Rep Power: 5
DnyanMiri is on a distinguished road
Hi Vinerm, you have been a source of great help. I was able to solve the problem of divergence in turbulent viscosity by keeping smallest cell volume greater than volume of the droplet.
Right now, as I start my simulation every parameter converges with time step of 10^-4 but after like 100 time steps continuity residual does not go below 10^-3. How can I solve this? any suggestions are welcomed.
I'm using SIMPLEC with second order schemes. Let me know if you need any more info.
Thank you!
DnyanMiri is offline   Reply With Quote

Old   June 15, 2020, 07:27
Default Continuity
  #13
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
Don't worry about that. 0.001 or 0.003 or even 0.005 are alright as long as there is good conservation of mass and energy as well as the monitors are stable.
DnyanMiri and Phanindra Raavi like this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Reply

Tags
boundary condition, fluent, heat flux, spray, temperature

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[OpenFOAM.org] compile error in dynamicMesh and thermophysicalModels libraries NickG OpenFOAM Installation 3 December 30, 2019 01:21
time step continuity problem in VAWT simulation lpz_michele OpenFOAM Running, Solving & CFD 5 February 22, 2018 20:50
Question about adaptive timestepping Guille1811 CFX 25 November 12, 2017 18:38
Radiation interface hinca CFX 15 January 26, 2014 18:11
Possible Bug in pimpleFoam (or createPatch) (or fluent3DMeshToFoam) cfdonline2mohsen OpenFOAM 3 October 21, 2013 10:28


All times are GMT -4. The time now is 02:04.